HEIDENHAIN CNC Pilot 4290 - Manual (Page 157)

HEIDENHAIN CNC PILOT 4290 145
Tapping G73
G73 cuts axial/radial threads using driven or stationary tools.
G73 is used for bore holes with contour definition (individual bore hole
or hole pattern) in the following program sections:
■ FRONT
■ REAR SIDE
■ SURFACE
The starting position is calculated from the safety distance and the
”run-in (slope) length B.”
Meaning of ”retraction length J”: Use this parameter for floating
tap holders. The cycle calculates a new nominal pitch on the basis of
the thread depth, the programmed pitch, and the ”retract length.” The
nominal pitch is somewhat smaller than the pitch of the tap. During
tapping, the drill is pulled away from the chuck by the ”retraction
length.” With this method you can acheive higher service life from the
taps.
Parameters
NS:
Contour block number with geometry of bore hole (G49, G300/
G310-Geo)
B: Slope length – default: Machining Parameter 7 ”Thread starting
length [GAL]”
S: Retraction speed – default: Tapping speed
K: Retraction plane (radial holes, holes in the YZ plane: diameter) –
default: to starting position or to safety clearance
J: Retraction length when using floating tap holders – default: 0
4.9 Dr
illing Cy
cles
Cycle run
1 Approach starting position at rapid traverse
according to ”K”:
■ K not programmed: Approach directly to starting
position.
■ K programmed: Approach to ”K,” and then to
starting position.
2 Move along ”slope length B” at feed rate
(synchronization of spindle and feed drives).
3 Cut the thread.
4 Returns at ”return speed S” according to ”K”:
■ K not programmed: Return to starting point.
■ K programmed: Return to position ”K.”
■ Hole pattern: NS refers to the bore hole
contour (and not the definition of the
pattern)).
■ ”Cycle stop” becomes effective at the
end of a thread cut.
■ Feed rate override is not in effect.
■ Do not use spindle override!